Gasket Bodies

Gasket joints are essential components in most structural assemblies. Gaskets as sealing components between structural components are usually very thin and made of various materials, such as steel, rubber and composites. From a mechanics perspective, gaskets act to transfer force between components. The primary deformation of a gasket is usually confined to one direction, namely, through thickness. The stiffness contributions from membrane (in plane) and transverse shear are much smaller in general compared to the through thickness.

A typical example of a gasket joint is in engine assemblies. A thorough understanding of the gasket joint is critical in engine design and operation. This includes an understanding of the behavior of gasket joint components themselves in an engine operation, and the interaction of the gasket joint with other components.

You can conveniently specify a solid body to be treated as a gasket by settings its Stiffness Behavior property to Gasket. You must also specify a material with a valid gasket model in Engineering Data.

The following restrictions apply to Gasket bodies:

The overall procedure for simulating gaskets in ANSYS Workbench is to run a Static Structural analysis and perform the following specialized steps:

  1. Specify a material with a valid gasket model in Engineering Data.

  2. Set the Stiffness Behavior of the Body object to Gasket. This produces a Gasket Mesh Control object beneath the Body object.

  3. Adjust Details view settings for the Gasket Mesh Control object and generate the mesh. See the Gasket Meshing section shown below.

  4. Specify the value for the Gasket Initial Gap property. The default value is 0. Valid entries must be greater than or equal to 0.

  5. Solve and review the gasket result. See the Gasket Results section for more information.

Gasket Meshing

A Gasket body is meshed with the INTER194 and INTER195 elements. The mesh will consist of a single layer of solid elements with all mid-side nodes dropped.

Upon specifying a gasket body, a Gasket Mesh Control object is added beneath the Body object in the tree. The Mesh Method property for the object is automatically set to Sweep and is read-only. By default, this property instructs the application to drop mid-side nodes on gasket element edges that are parallel (Normal To) to the scoped sweep direction. You may wish to refer to the Sweep Method Control section of the Meshing User's Guide for additional information about this property. The Gasket Mesh Control operates in the same fashion.

To use gasket element meshing after setting the 3D Body object's Stiffness Behavior to Gasket:

  1. If desired, you can change the setting of the Free Face Mesh Type property. Options include All Quad, Quad/Tri (default), or All Tri.

  2. The Mesh Method is automatically set to Sweep and is read-only.

  3. The Element Order property is set to Use Global Setting by default. This setting (as well as the Quadratic setting) results in quadratic elements with midside nodes to be dropped in the normal direction. When Element Order is set to Linear, the midside nodes are dropped, resulting in linear elements.

  4. Src/Trg Selection is set to Manual Source. These are the default settings.

  5. Select a Source face. The selected face must lie on the gasket body.

  6. The Target selection is Program Controlled by default. If desired, you can set Src/Trg Selection to Manual Source and Target. You can then choose a Target face manually.


Note:  Mesh object property changes affect the of the Gasket Mesh Control object.


When generating the gasket element mesh, the application drops the midside nodes on the edges that are parallel to the sweep direction. For example, consider the mesh shown below. To define the sweep method, Src/Trg Selection was set to Manual Source; one face (the “top” face) was selected for Source. In the resulting mesh, the gasket element faces on the source and target are quadratic, but the faces on the sides are linear.

Gasket Results

Specialized results are available for analyzing gaskets. See Gasket Results for details.


Release 18.2 - © ANSYS, Inc. All rights reserved.